gglines wrote:

I'll be cutting pockets in 6061 aluminum and want to mill the bottoms as
smoothly as possible to cut down on finishing steps. Any recommended end
mills? The pockets will be 1" wide by 8" long by 1/4" deep.


The size of the end mill is limited by the corner radius of your pockets.
But, you want to use the largest end mill you can, as it will be stiffer
than a thin one. The smaller end mills deflect more when cutting, and
the tip of the flutes leave gouges in the bottom. A stub end mill is
stiffer than a regular length of cut version. Since your pocket is only
1/4" deep, that may help. 4-flute end mills are a little stiffer than
2-flute. Solid carbide end mills are astoundingly stiffer than HSS.

Coolant may be a big help. When doing a lot of metal removal in
a small area, the workpiece heats up, and aluminum will make a big
mess all over the cutter if it gets too hot.

If you want a very smooth bottom with minimal tracks on it, you will
need a VERY tight machine. Finishing the entire pocket to full dimensions
except leaving a little material (.005 - .010") on the bottom, and then
making a finishing pass to remove that last bit of metal may be needed
to reduce the visible tracks.

Jon

"Jon Elson" wrote in message
...


gglines wrote:

I'll be cutting pockets in 6061 aluminum and want to mill the bottoms as
smoothly as possible to cut down on finishing steps. Any recommended end
mills? The pockets will be 1" wide by 8" long by 1/4" deep.


The size of the end mill is limited by the corner radius of your pockets.
But, you want to use the largest end mill you can, as it will be stiffer
than a thin one. The smaller end mills deflect more when cutting, and
the tip of the flutes leave gouges in the bottom. A stub end mill is
stiffer than a regular length of cut version. Since your pocket is only
1/4" deep, that may help. 4-flute end mills are a little stiffer than
2-flute. Solid carbide end mills are astoundingly stiffer than HSS.

Coolant may be a big help. When doing a lot of metal removal in
a small area, the workpiece heats up, and aluminum will make a big
mess all over the cutter if it gets too hot.

If you want a very smooth bottom with minimal tracks on it, you will
need a VERY tight machine. Finishing the entire pocket to full dimensions
except leaving a little material (.005 - .010") on the bottom, and then
making a finishing pass to remove that last bit of metal may be needed
to reduce the visible tracks.

Jon


Yep! What Jon said, and I'd add to it to run the spindle as fast as you
can. You can run a 1" end mill at 4,200 RPM in aluminum and get
outstanding results. Use kerosene to lube the cut if you don't have
anything else in mind. Brush applying it works great, especially in a
cavity. If you have the option, when you take your finish cut, if you
have to offset the table to get proper width, make sure you climb mill.
That, in aluminum, leaves a wonderful finish, especially if you're
lubricating the cut well.

Good luck~

Harold

Harold & Susan Vordos wrote:

"Jon Elson" wrote in message
...


gglines wrote:

I'll be cutting pockets in 6061 aluminum and want to mill the bottoms as
smoothly as possible to cut down on finishing steps. Any recommended end
mills? The pockets will be 1" wide by 8" long by 1/4" deep.


The size of the end mill is limited by the corner radius of your pockets.
But, you want to use the largest end mill you can, as it will be stiffer
than a thin one. The smaller end mills deflect more when cutting, and
the tip of the flutes leave gouges in the bottom. A stub end mill is
stiffer than a regular length of cut version. Since your pocket is only
1/4" deep, that may help. 4-flute end mills are a little stiffer than
2-flute. Solid carbide end mills are astoundingly stiffer than HSS.

Coolant may be a big help. When doing a lot of metal removal in
a small area, the workpiece heats up, and aluminum will make a big
mess all over the cutter if it gets too hot.

If you want a very smooth bottom with minimal tracks on it, you will
need a VERY tight machine. Finishing the entire pocket to full dimensions
except leaving a little material (.005 - .010") on the bottom, and then
making a finishing pass to remove that last bit of metal may be needed
to reduce the visible tracks.

Jon


Yep! What Jon said, and I'd add to it to run the spindle as fast as you
can. You can run a 1" end mill at 4,200 RPM in aluminum and get
outstanding results. Use kerosene to lube the cut if you don't have
anything else in mind. Brush applying it works great, especially in a
cavity. If you have the option, when you take your finish cut, if you
have to offset the table to get proper width, make sure you climb mill.
That, in aluminum, leaves a wonderful finish, especially if you're
lubricating the cut well.

Good luck~

Harold

Good advice. Use a stone to put a slight radius on the tips of your tool.
Something on the order of .005-.015, depending on size of cutter. Make sure to
keep relief behind the leading edge, don't flatten it out when stoning or your
tool will rub and trash your finish. Keep chips cleared away so they don't get
pulled back through your cut, they have no good business in there. And kerosene
is "the bomb" if you can stand the smell and getting it on you. I worked on a
job in early 70s that was run with a 50/50 kero-cutting oil mix. Early tape
reading NC machine with multiple fixture positions, looping cycle with no stop,
had to move parts through progression while it ran, and no splashguards. I do
not have any kerosene in my shop, I will use other things, thankyou.

michael

In article , Harold & Susan Vordos wrote:

Yep! What Jon said, and I'd add to it to run the spindle as fast as you
can.

I should have kept reading. Between you and Jon you covered everything
that I said.

If you have the option, when you take your finish cut, if you
have to offset the table to get proper width, make sure you climb mill.

I'm glad you put that 'if' in there, 'cause it's a doozie... I've wrecked
parts by thinking I could get away with a few-thou climb mill on a
bridgeport.... Sometimes it works, and sometimes... BANG!!! 8-/

--
=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-
Mike Graham | Metalworker, rustic, part-time zealot.
|
http://www.metalmangler.com| Caledon, Ontario, Canada

Mike Graham wrote in message ...
In article , Harold & Susan Vordos
wrote:

Yep! What Jon said, and I'd add to it to run the spindle as fast as you
can.

I should have kept reading. Between you and Jon you covered everything
that I said.

If you have the option, when you take your finish cut, if you
have to offset the table to get proper width, make sure you climb mill.

I'm glad you put that 'if' in there, 'cause it's a doozie... I've wrecked
parts by thinking I could get away with a few-thou climb mill on a
bridgeport.... Sometimes it works, and sometimes... BANG!!! 8-/


Mike, could you tell us what the potential problems are when climb milling
the last few thou ?

Thanks
Michael no xx's in address

=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-
Mike Graham | Metalworker, rustic, part-time zealot.
|
http://www.metalmangler.com| Caledon, Ontario, Canada

On Wed, 27 Aug 2003 13:42:41 GMT, "Michael Cameron"
wrote:

Mike, could you tell us what the potential problems are when climb milling
the last few thou ?


If you have five or ten thousandths of play (at the feed dial) when
you reverse the lead screw and are climb milling, it means that if the
cutting edge generates enough pulling forces the table will jump the
five or ten thou all at once. So the chip thickness and cutting load
skyrockets.

To see how much free play you have, move the table with the feedscrew
stopping on "0", then turn the screw the opposite direction just until
the table moves and note the reading again. It is not unusual to find
20 to 50 thou or more on a perfectly useable machine. And the
distance will increase and decrease as you go towards and away from
the most used (worn) part of the screw.

You can put a light drag on the table with the clamping screw on the
feed axis to help minimize the danger of it self feeding but that also
increases the feed forces and the wear on the screws.

I often would take a normal, non-climb, cut and then simply stop and
climb feed back to the start to clean up a cut. The loading in the
cut and spring in the tool will usually give you a light cut. If you
are not finishing off the material (like in a pocket) you have to be
careful that you don't come back too far.

Climb cutting can make an incredible difference in the surface finish
and appearance.



-----= Posted via Newsfeeds.Com, Uncensored Usenet News =-----
http://www.newsfeeds.com - The #1 Newsgroup Service in the World!
-----== Over 100,000 Newsgroups - 19 Different Servers! =-----

In article , Michael Cameron wrote:

Mike, could you tell us what the potential problems are when climb milling
the last few thou ?

Jack covered the issue nicely. I once had a head crash with a 3/4"
roughing endmill that resulted in the head getting tilted 10 degrees.
That's a pretty serious crash. The part was junk after that.
As Jack said, normally you're okay to climb mill over what you're already
conventionally milled at the same setting. Normally.

--
=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-
Mike Graham | Metalworker, rustic, part-time zealot.
|
http://www.metalmangler.com| Caledon, Ontario, Canada

Great advice, thanks all!

George